Latch Spring. Problem:

Transcription

1 Problem: Shown in the figure is a 12-gauge ( in) by 3/4 in latching spring which supports a load of F = 3 lb. The inside radius of the bend is 1/8 in. Estimate the stresses at the inner and outer surfaces at the critical section. Joseph Shigley and Charles Mischke. Mechanical Engineering Design 5th ed. New York: McGraw Hill, May 2002.

2 Overview Anticipated time to complete this tutorial: 1 hour Tutorial Overview This tutorial is divided into six parts: 1) Tutorial Basics 2) Starting Ansys 3) Preprocessing 4) Solution 5) Post-Processing 6) Hand Calculations Audience This tutorial assumes minimal knowledge of ANSYS 8.0; therefore, it goes into moderate detail to explain each step. More advanced ANSYS 8.0 users should be able to complete this tutorial fairly quickly. Prerequisites 1) ANSYS 8.0 in house Structural Tutorial Objectives 1) Model the the latch spring in ANSYS 8.0 2) Analyze the latch spring for the stresses at the inner and outer surfaces of the critical section Outcomes 1) Learn how to start Ansys 8.0 2) Gain familiarity with the graphical user interface (GUI) 3) Learn how to create and mesh a simple geometry 4) Learn how to apply boundary constraints and solve problems 2

3 In this tutorial: Instructions appear on the left. Latch Spring Visual aids corresponding to the text appear on the right. Tutorial Basics All commands on the toolbars are labeled. However, only operations applicable to the tutorial are explained. The instructions should be used as follows: Bold > Example: Italics MB1 MB2 MB3 Text in bold are buttons, options, or selections that the user needs to click on > Preprocessor > Element Type > Add/Edit/DeleteFile would mean to follow the options as shown to the right to get you to the Element Types window Text in italics are hints and notes Click on the left mouse button Click on the middle mouse button Click on the right mouse button Some basic ANSYS functions are: To rotate the models use Ctrl and MB3. To zoom use Ctrl and MB2 and move the mouse up and down. To translate the models use Ctrl and MB1. 3

4 Starting Ansys For this tutorial the windows version of ANSYS 8.0 will be demonstrated. The path below is one example of how to access ANSYS; however, this path will not be the same on all computers. For Windows XP start ANSYS by either using: > Start > All Programs > ANSYS 8.0 > ANSYS or the desktop icon (right) if present. Note: The path to start ANSYS 8.0 may be different for each computer. Check with your local network manager to find out how to start ANSYS

5 Starting Ansys Once ANSYS 8.0 is loaded, two separate windows appear: the main ANSYS Advanced Utility Window and the ANSYS Output Window. The ANSYS Advanced Utility Window, also known as the Graphical User Interface (GUI), is the location where all the user interface takes place. Graphical User Interface Output Window The Output Window documents all actions taken, displays errors, and solver status. 5

6 Starting Ansys The main utility window can be broken up into three areas. A short explanation of each will be given. First is the Utility Toolbar: From this toolbar you can use the command line approach to ANSYS and access multiple menus that you can t get to from the main menu. Note: It would be beneficial to take some time and explore these pull down menus and familiarize yourself with them. Second is the ANSYS Main Menu as shown to the right. This menu is designed to use a top down approach and contains all the steps and options necessary to properly preprocess, solve, and postprocess a model. Third is the Graphical Interface window where all geometry, boundary conditions, and results are displayed. The tool bar located on the right hand side has all the visual orientation tools that are needed to manipulate your model. 6

7 Starting Ansys With ANSYS 8.0 open select > File > Change Jobname and enter a new job name in the blank field of the change jobname window. Enter the problem title for this tutorial. In order to know where all the output files from ANSYS will be placed, the working directory must be set in order to avoid using the default folder: C:\Documents and Settings. > File > Change Directory > then select the location that you want all of the ANSYS files to be saved. Be sure to change the working directory at the beginning of every problem. With the jobname and directory set the ANSYS database (.db) file can be given a title. Following the same steps as you did to change the jobname and the directory, give the model a title. 7

8 To begin the analysis, a preference needs to be set. > Main Menu > Preferences Preprocessing Place a check mark next to the Structural box. This determines the type of analysis to be performed in ANSYS. >Ok The ANSYS Main Menu should now be opened. Click once on the + sign next to Preprocessor. > Main Menu > Preprocessor The Preprocessor options currently available are displayed in the expansion of the Main Menu tree as shown to the right. 8

9 Preprocessing As mentioned previously, the ANSYS Main Menu is designed in such a way that one should start at the beginning and work towards the bottom of the menu in preparing, solving, and analyzing your model. Note: This procedure will be shown throughout the tutorial. Select the + next to Element Type or click on Element Type. The extension of the menu is shown to the right. > Element Type Select Add/Edit/Delete and the Element Type window appears. Select add and the Library of Element Types window appears. > ADD/EDIT/DELETE > Add In this window, select the types of elements to be defined and used for this problem. For this model Tet 10node 187 elements will be used. > Solid > Tet 10node 187 In the Element Types window Type 1 Solid187 should be visible signaling that the element type has been chosen. Close the Element Types window. > Close 9

10 Preprocessing The properties for the Solid187 elements need to be chosen. No real constants need to be defined, but material properties do. The material properties for the Solid187 elements need to be defined. > Preprocessor > Material Props > Material Models The Define Material Models Behavior window should now be open. This window has many different possibilities for defining the materials for your model. We will use set the isotropic linearly elastic structural properties. Select the following from the Material Models Available window: > Structural > Linear > Elastic > Isotropic The window titled Linear Isotropic Properties for Material Number 1 now appears. This window is the entry point for the material properties to be used for the model. Enter 30e6 (30 Mpsi) in for EX (Young's Modulus) and 0.3 for PRXY (Poisson's Ratio). Close the Define Material Model Behavior window. > Material > Exit 10

11 Preprocessing The next step is to define the keypoints (KP s) where loads and constraints will be applied: > Preprocessor > Modeling > Create > Keypoints > In Active CS The Create Keypoints in Active CS window will now appear. Here the KP s will be given numbers and their respective (XYZ) coordinates. Enter the KP numbers and coordinates for the pin definition. Select Apply after each KP has been defined. Note: Be sure to change the keypoint number every time you click apply to finish adding a keypoint. If you don t it will just move the last keypoint you entered to the new coordinates you just entered. KP # 1: X=0, Y=0, Z=0 KP # 2: X=0.1094, Y=0, Z=0 KP # 3: X=0, Y=0, Z=0.75 KP # 4: X=0.1094, Y=0, Z=0.75 KP # 5: X=0, Y=1.25, Z=0.75 KP # 6: X=-0.125, Y=1.375, Z=0.75 KP # 7: X=-4.125, Y=1.375, Z=0.75 Select Ok when complete. In the case that a mistake was made in creating the keypoints, select: > Preprocessor > Modeling > Delete > Keypoints Select the inappropriate KP s and select OK. The created KP s should look similar to the example to the right (note: the window is rotated slightly). 11

12 At times it will be helpful to turn on the keypoint numbers. > PlotCtrls > Numbering > put a checkmark next to keypoint numbers Other numbers (for lines, areas, etc..) can be turned on in a similar manner. Latch Spring Preprocessing The next step is to create lines between the KP s. > Preprocessor > Modeling > Create > Lines > Lines > Straight Lines The Create Straight Lines window should appear. You will create 5 lines. Create line 1 between the first two keypoints. For line 1: MB1 KP 1 then MB1 KP 2. The other lines will be created in a similar manner. Rotate the screen if needed to aid in creating the lines. For line 2: MB1 KP 1 then MB1 KP 3. For line 3: MB1 KP 3 then MB1 KP 4. For line 4: MB1 KP 4 then MB1 KP 2. For line 5: MB1 KP 3 then MB1 KP 5. For line 5: MB1 KP 6 then MB1 KP 7. Verify that each line only goes between the specified keypoints. When you are done creating the lines click ok in the Create Straight Lines window. If you make a mistake, use the following to delete the lines: > Preprocessor> Modeling > Delete > Lines Only 12

13 If while working, the geometry you created disappears select from the Utility Toolbar. > Plot > Multi-Plots Latch Spring Preprocessing Other items (lines, areas, volumes, elements, keypoints, nodes..) can be plotted in the window in a similar manner. An arc needs to be created between KP 6 and KP 5. > Preprocessor > Modeling > Create > Lines > Arcs > By End KPs & Rad Select KP 6 and KP 5 for the start and ending keypoints by using MB1. Select KP 3 as the reference for the center of curvature side. Type for the radius of the arc in the Arc by End KPs & Radius box that is now displayed. Rotate the model so that all of the lines can be seen. 13

14 An area will now be created that can be extruded to finish up the geometry. > Preprocessor > Modeling > Create > Areas > Arbitrary > By Lines Latch Spring Preprocessing Select the four lines at that the bottom of the screen that create a rectangular area. (The four lines are near the origin marker.) The new area is now filled in as shown to the right. This area will now be extruded along the other three lines. > Preprocessor > Modeling > Operate > Extrude > Areas > Along Lines Select the area just created. (In the Sweep along lines box) Select the three lines not used to create the area. > OK The geometry is now complete. 14

15 Preprocessing Before the model can be meshed for solving, a hard point will be added so that the force can be applied to the middle of the latch. > Preprocessor > Modeling > Create > Keypoints > Hard PT on line > Hard PT by ratio Select the top line at the end of the latch where the force will be applied. (In the Hard PT by ratio window) In the Create Hard PT by Ratio window, enter 0.5 as the length ratio. The model will be meshed by first setting a size control for the elements and then meshing the geometry. > Preprocessor > Meshing > Size Cntrls > ManualSize > Global > Size In the Global Element Sizes window set the element edge length to 0.05 and leave the No. of element divisions set at zero. To mesh the model. > Preprocessor > Meshing > Mesh > Volume > Free In the Mesh Volumes window select Pick All. > Pick all The model is meshed and ready for constraints and the load to be added. 15

16 We will now move into the solution phase. Latch Spring Solution Before applying the loads and constraints to the latch, we will select to start a new analysis: > Solution > Analysis Type > New Analysis For type of analysis select Static and select Ok. The constraints will now be added. For this problem, constraints must be added to fix the latch as it would be if it were attached to a wall with two bolts. To apply constraints select: > Solution > Define Loads > Apply > Structural > Displacement > On Areas Select the area that represents where the latch would be attached to the wall as shown in purple below. 16

17 Solution In the Apply U,ROT on Areas window select All DOF. The 3 lb load will now be added. > Solutions > Define Loads > Apply > Structural > Force/Moment > On Keypoints Select the hard point that was previously created on the top of the latch at its end. In the Apply F/M on KPs window select FY as the Direction of force/mom. Type -3.0 for the Force/moment value. The model is ready to be solved. 17

18 Solution The next step in completion of the tutorial is to solve the current load step that has been created. Select: > Solution > Solve > Current LS The Solve Current Load Step window will appear. To begin the analysis select Ok. The analysis should begin and when the solution is done a Note window should appear that states the analysis is complete. Note: Depending on the speed of your computer, it may be several minutes before the solution is complete. Close both the Note window and /STATUS Command window. 18

19 Results are viewed by using post processing commands. Post Processing From the ANSYS Main Menu select: > General Postproc > Results Viewer In the Results Viewer select the down arrow next to Choose a result item and select: > Nodal Solution > Stress > Von Mises Stress MB1 the Plot Results button to see the results for the Von Mises Stresses. Use the query tool to find the stresses at the inner and outer radius. If you hold down MB1 with the query tool active and move it over the part you can see values in many locations quickly. The highest values for the inner radius (shown in red) range from 10,000 to 10,500 psi, with an average value of 10,250 psi. The highest stress values range for the outer radius range from about 6,300 to 6,600 psi (excluding the edges). The values are in the ballpark of the closed form solution shown on the next page. This model assumes that the part of the latch that touches the wall does not take any of the stress (its dark blue color indicates basically no stress). In real life, this section would take some of the stress as it bends away from the wall. A more challenging and accurate model would have included the bolt holes and the latches attachment to the wall with these bolts. In FEA, it is a good idea to make assumptions to simplify the model, and then, if they adversely affect the solution, you can always go back and include them in the model. 19

20 Hand Calculations r o = radius of outer fiber r i = radius of inner fiber h = depth of section c o = distance from neutral axis to outer fiber c i = distance from neutral axis to inner fiber r n = radius of neutral axis R = radius of centroidal axis e = distance from centroidal axis to neutral axis A = area of cross section M = moment ri = 0.125in ro = = in h R = r i + 2 h rn = ln( ro / ri ) R = / 2 = in rn = / ln(0.2344/ 0.125) = in e = R rn = = in ci = rn ri = = in co = ro rn = = in A = 0.75(0.1094) = in 2 M = Force(4 + h / 2) = 3( / 2) = 12.16in lb F σ Mci i = A Aeri (0.049) σi = = 10,200psi ( )0.125 σo = F A σi = Mc o Aero (0.060) 0.082( ) = 6630psi 20